Trochoidal feed versus traditional on high feed mill + serious warning about G1 ,R

Tichy · May 1, 2019

First of all the warning. I am unsure if this is is specific to my machine, if something is wrong, but here goes.

I totaled a high feed face mill half a year ago. This was done by issuing the following type of code:

G1 Y100 ,R10
X100

As I recall the piece was firmly, firmly secured. I thought maybe it wasn't, but yesterday it happened again with my 80MM regular face mill (KSOM, 42 degree inserts or so, very fast) and the same type of movement. Thankfully it survived.

The result of the move using the 50MM high feed mill was, eh, dramatic. The workpiece was maybe 20kg P2. It just flipped over, right out of the vise and crashed into the spindle. The one I worked with yesterday apparently wanted to do the same, but it was stopped by a very durable material stop I had mounted on the left side of the piece, with the result that this stop was instead bent. Checking the vise, the screw securing it was still tightened and hard to untight.

So something is funky with that ,R option. For now I will avoid ever using it again. Opinions welcome.

The second thing is this: When using my high feed mill in full contact with the material (80% Ae or so,) I may have F'n'S at say Vc190 F0.8 and Ap 1.15mm. Translating it ending up at F5000-6000 or so. My G0 feed rate is 15000.

What would I then use for a trochoidal feed rate and how big an Ae would be recommended? We're talking 10' angle high feed mill.

Vancbiker · May 1, 2019

Tichy said:
.....So something is funky with that ,R option. For now I will avoid ever using it again. Opinions welcome......

Control you are using would be helpful. Also, has the ,R function always caused trouble or just randomly? If random, then posting the actual code, several lines before and after the crash move would be good.

I use ,R on my Mitsu control nearly every time I finger CAM a program and it always works unless I make a mistake. Then it just raises an alarm and stops feeding.

Tichy · May 1, 2019

Vancbiker said:
Control you are using would be helpful. Also, has the ,R function always caused trouble or just randomly? If random, then posting the actual code, several lines before and after the crash move would be good.

I use ,R on my Mitsu control nearly every time I finger CAM a program and it always works unless I make a mistake. Then it just raises an alarm and stops feeding.

Fanuc 21i.

It's always been funky. It works when you go slow, but the control seems to stutter a bit performing the move, and with feeds I run in production that's disaster.

Never noticed the same behavior with G2 or G3.

Qwan · May 2, 2019

Tichy said:
First of all the warning. I am unsure if this is is specific to my machine, if something is wrong, but here goes.

I totaled a high feed face mill half a year ago. This was done by issuing the following type of code:

G1 Y100 ,R10
X100...

Did you create the program in your cam system or manually create it?

If you created it in cam, can you simulate it? You might be surprised what you find. Some users don't like to simulate their small programs but in reality they simulate fast and and the value is high. Even higher if the parts run is long or if a single part is worth a lot of money.

countryboy1966 · May 4, 2019

I'm curious as I believe I'm ignorant to what the R value signifies in this event. What is the machine supposed to do with this line of code?

Also - With no feed number present in the specific line doesn't it revert to the last feed rate value specified?

Is it possible that although the cuttter can handle it, the load is so great on the part that tool load exceeds work holding force especially depending on feed direction and work holding design?

gregormarwick · May 4, 2019

I thought that G1 R was a (fanuc) lathe thing. Is it definitely supported on M controls too?

I've never seen it used on a mill.

TeachMePlease · May 4, 2019

gregormarwick said:
I thought that G1 R was a (fanuc) lathe thing. Is it definitely supported on M controls too?

I've never seen it used on a mill.

G1 R, A, C all work on my Mits Meldas lathe controls.

gregormarwick · May 4, 2019

TeachMePlease said:
G1 R, A, C all work on my Mits Meldas lathe controls.

That's why I put Fanuc in brackets. I haven't used too many different lathe controls, but of the ones I have used, only Fanuc do that.

But on a mill??

angelw · May 4, 2019

gregormarwick said:
I thought that G1 R was a (fanuc) lathe thing. Is it definitely supported on M controls too?

I've never seen it used on a mill.

Hello Gregor,
Most definitely supported on Fanuc M controls, but it is an Option Feature "Angle Chamfering and Corner Rounding". It follows all the same rules that apply when used on a Lathe Control.

Other usual suspects, such as HAAS, Mazak (EIA Programming), Meldas etc, all have the same feature available and use the same syntax.

Regards,

Bill

gregormarwick · May 4, 2019

angelw said:
Hello Gregor,
Most definitely supported on Fanuc M controls, but it is an Option Feature "Angle Chamfering and Corner Rounding". It follows all the same rules that apply when used on a Lathe Control.

Other usual suspects, such as HAAS, Mazak (EIA Programming), Meldas etc, all have the same feature available and use the same syntax.

Regards,

Bill

Thanks for clearing that up Bill

litlerob1 · May 5, 2019

While Gregor and Bill are satisfied, I remain in the dark. Why is the OP using G1 R* for Milling?

R

Delw · May 5, 2019

litlerob1 said:
While Gregor and Bill are satisfied, I remain in the dark. Why is the OP using G1 R* for Milling?

R

you and me both, I am hoping Bill could give an example. it sounds interesting. I understand the part about the R,(equals radius just not the

G1 Y100 ,R10
X100

this program baffles me. it uses a "comma" ?

does this code start at y100 then run a r10 rad all the way to the x100 point?
basically a straight line in circles (Trochoidal )?

rcs60 · May 5, 2019

Fanuc allows the use of ,R to put a radius at the intersection of the 2 lines also ,C (they are options)

it would be like programming
G1X0.
G1Y90
G2X10.Y100I0.J-10(OR G3X10.Y100R10.)
G1X100.

the thing i would watch for is the speed that may occur going around the corner with the end mill
with cutter comp enabled it may actually increase the feed to compensate for the corner at the speed programmed Depending on how the control is configured to act

angelw · May 5, 2019

litlerob1 said:
While Gregor and Bill are satisfied, I remain in the dark. Why is the OP using G1 R* for Milling?

R

Hello Rob,
Not really satisfied, just confirming that the "Angle Chamfering and Corner Rounding" option is available on Mill Controls, not only Lathe Controls. Hell, I don't even like using R Format for Circular Interpolation because if either the Start, or End Coordinates are incorrect, the Circular Move will still execute without error, if its geometrically possible to construct said arc between the points given. This can lead to such an error not being picked up until after the part is cut an thorough inspection is carried out and may result is an expensive, well machined piece of scrap.

Delw said:
you and me both, I am hoping Bill could give an example. it sounds interesting. I understand the part about the R,(equals radius just not the

G1 Y100 ,R10
X100

this program baffles me. it uses a "comma" ?

does this code start at y100 then run a r10 rad all the way to the x100 point?
basically a straight line in circles (Trochoidal )?

Hello Delw,
This is a feature more to aid the Finger CAMist. Writing a Post for CAM software to use this option would be a bitch.

Following is the code for the part profile picture below with Sequence Numbers included so as to be able to relate it to the picture. This is an example from a Fanuc Mill Operator's Manual.

N001 G92 G90 X0 Y0
N002 G00 X10.0 Y10.0
N003 G01 X50.0 F10.0 ,C5.0
N004 Y25.0 ,R8.0
N005 G03 X80.0 Y50.0 R30.0 ,R8.0
N006 G01 X50.0 ,R8.0
N007 Y70.0 ,C5.0
N008 X10.0 ,C5.0
N009 Y10.0
N010 G00 X0 Y0

What Tichy is doing is advancing the Start of the Circular Move with a Linear Move. At best this is pseudo Trochoidal, its not a Trochoidal path.

Regards,

Bill

Delw · May 5, 2019

angelw said:
Hello Rob,
Not really satisfied, just confirming that the "Angle Chamfering and Corner Rounding" option is available on Mill Controls, not only Lathe Controls. Hell, I don't even like using R Format for Circular Interpolation because if either the Start, or End Coordinates are incorrect, the Circular Move will still execute without error, if its geometrically possible to construct said arc between the points given. This can lead to such an error not being picked up until after the part is cut an thorough inspection is carried out and may result is an expensive, well machined piece of scrap.

Hello Delw,
This is a feature more to aid the Finger CAMist. Writing a Post for CAM software to use this option would be a bitch.

Following is the code for the part profile picture below with Sequence Numbers included so as to be able to relate it to the picture. This is an example from a Fanuc Mill Operator's Manual.

N001 G92 G90 X0 Y0
N002 G00 X10.0 Y10.0
N003 G01 X50.0 F10.0 ,C5.0
N004 Y25.0 ,R8.0
N005 G03 X80.0 Y50.0 R30.0 ,R8.0
N006 G01 X50.0 ,R8.0
N007 Y70.0 ,C5.0
N008 X10.0 ,C5.0
N009 Y10.0
N010 G00 X0 Y0

View attachment 255916

What Tichy is doing is advancing the Start of the Circular Move with a Linear Move. At best this is pseudo Trochoidal, its not a Trochoidal path.

Regards,

Bill

Thanks alot now I understand. thats actually pretty cool not what I thought it was but still pretty cool, been programing for 30+ years and never knew you could do that. learn something everyday.

Thanks Again

Vancbiker · May 5, 2019

Not very often is this option purchased by a buyer or spec'd by the machine builder for machining centers IME. I have it on my home shop Mori though. Don't do too many finger CAM programs, but when I do I use ,R on almost all G1 moves.

litlerob1 · May 5, 2019

Okay, I accept that. When you program linear paths, and there is an XY intersection you can add an "R" vlaue to create and arc at the intersection, great. But it doesn't explain why R would make a Tool crash or a part come out of a vise.

The Thread title is a warning against using R.

Vancbiker · May 6, 2019

litlerob1 said:
.... But it doesn't explain why R would make a Tool crash or a part come out of a vise.

The Thread title is a warning against using R.

Yep, that's why I asked for more details early on.

I have not used ,R on a 21M, and do not have access to one to test, but it has always worked on any flavor of Fanuc I have tried. The OP does mention a "stutter" on the radius move when using a high feedrate. The 21M is the low end control of the 16,18,21 family. Not sure about a "stutter", but could accept that the control might "hesitate" a moment while processing the combination movement.

Honestly, I think he is mistakenly thinking something the ,R function is responsible when some other problem resulted in kicking a part out of the vise.

Tichy · May 8, 2019

Vancbiker said:
Yep, that's why I asked for more details early on.

I have not used ,R on a 21M, and do not have access to one to test, but it has always worked on any flavor of Fanuc I have tried. The OP does mention a "stutter" on the radius move when using a high feedrate. The 21M is the low end control of the 16,18,21 family. Not sure about a "stutter", but could accept that the control might "hesitate" a moment while processing the combination movement.

Honestly, I think he is mistakenly thinking something the ,R function is responsible when some other problem resulted in kicking a part out of the vise.

Actually I have seen the stutter for myself. Say you have a part x100 y100 and you wanna contour it origo upper left with a 5mm corner radius.

Code:

x0 y50
g3 x0y0r25 (R in G3 works fine at my machine.)
g1x100,r5
y-100,r5
x0,r5
y0,r5
x10
g3y50r25

I can visually see the pause/"stutter" when the control is performing the ,R move. Slow feed this is no problem. ,C works fine. Thinking if G8 might fix it but I'm unsure of the parameters involved (as in what they do and what'd be recommended.)

This latest part we're talking about was brutally well-fastened and the DOC was only 2mm.

litlerob1 · May 8, 2019

Tichy, that doesnt explain why it threw a part.

R

BTW using R in an Arc move G2 and G3 is standard, for defining the center of the Arc. Using it in G1 is not a regular practice.

Trochoidal feed versus traditional on high feed mill + serious warning about G1 ,R

Aluminum

Diamond

Aluminum

Cast Iron

Hot Rolled

Diamond

Diamond

Diamond

Diamond

Diamond

Diamond

Stainless

Plastic

Diamond

Stainless

Diamond

Diamond

Diamond

Aluminum

Diamond

Similar threads